How To Model a Wheel in Fusion 360 - Day 10

hello and welcome to day number 10 and this is the day where i finally start modelling the first parts of the salva lk 7. it took me nine videos to get to a point where i feel confident enough to use the tourist in fusion 360 and actually build something and as you can see i've started to recreate or rebuild the wheel according the reference images and i've also already placed the wheel in our main assembly and while i was doing my research i came across a reference image it was this one here that attracted my attention um the version of the vehicle that you can see here was one that was taken by the british army and shipped over to the us during the world war ii and the us army made some tests with it to find out how the vehicle works and for this reason they have attached a different set of wheels and i think these wheels look much better than the original wheels that are attached to the rk7 so i have decided to give it a try and recreate these wheels instead and in the next 20 minutes i'm gonna show you exactly and step by step how i built the rim the tire and the thread pattern now let's get started as you can see i've already placed a circle in the scene this one serves as a guideline it helps me to get an idea of how big the final wheel should be and before i start drawing the first sketch lines let's create two new components first so i'll go to assembly new component the first one is my rim and the second one and before i create this one i make sure that the top level assembly is active i go to assembly drop down menu again new component this one is my entire component and before i continue with the rim i make sure that the corresponding component is active then let's choose the right plane first then i hit l on the keyboard to enter the sketch mode pick the right plane zoom in a little bit and draw a line like so and when i do this you can see that this purple line appears and this is a projection of our circle and this happens automatically because i've set the settings under preferences if you go to design here the outer project edges and references is checked and whenever this one is on everything you touch with the line gets automatically projected to the currently active sketch plane so you can turn this off if you don't want a fusion to project all of your lines then i simply continue to add an additional line like so and one more and then let's draw another line at the top this is going to be another reference line and i click on it hit the x key on the keyboard to turn it into a construction line and give it some dimensions with the d key let's probably set this to 20 centimeters and then i'm gonna use the coincident constraint to click on this purple circle first and then i hover over the construction line by holding down the shift key to select the center point and now this line is constrained to the center and i'm going to use this to determine the width of the wheel so let's make these lines a little bit narrower i'm just eyeballing here of course it's always a good idea to turn your sketches into fully defined sketches but for this demonstration it's not necessary also for the entire design it wasn't necessary to define every line perfectly because the main focus was more on the the actual look and the forms of the wheel then i'm gonna replace this straight line with an arc so i simply select and delete it then i press s on the keyboard type in arc to select the three point arc 0.1.2 and 0.3 somewhere in the middle and then let me quickly adjust the lines a little bit and probably make this a little bit higher and a little bit wider and then i select all of the line segments press o on the keyboard to bring up the offset tool and then let's offset this one by minus one and then i i'm gonna close the profile with the line tool again double click to select all of the outlines and then i mirror it by selecting the center line and finish the sketch and we can now already try to revolve the profile so i choose the revolve feature select both profiles and the axis around here and this already turns our simple sketch into the base of the rim it's probably a little bit too white so i'm gonna show the sketch double click on the sketch icon to enter the sketch let's see if we can move the whole thing down just a tad exit the sketch again and this already looks a lot better now let's continue with the inner part of the rim and for this reason i deactivate the auto projection of the reference lines first i'm going to design and turn off the auto project edges on references and then i select the right plane again press the l key to start the sketch tool select the right plane and before i start sketching let's slice the thing so that we can see what's going on a little bit easier then i simply start drawing some lines then i switch to the three point arc tool one more time draw an arc around here and then another straight line at the bottom and i select this hit x on the keyboard to turn it into a construction line then i select the arc and the construction line and make both tangent and then i simply continue with the line tool and draw a few more lines like so and now let's select the segments by double clicking on them press o on the keyboard to bring up the offset command then i'm going to offset it by -1 and last but not least i'm gonna close the profile then i'm drawing a horizontal line straight through the other line and trim these parts away and close the profile at the bottom and then we can already try to revolve also this one so go to create revolve select the profile and instead of a new body i want to join it with the part of the rim that i've created before select the y-axis again and press ok this looks already quite good so let's do some minor adjustments i'm gonna double click on the sketch profile again enable slice and again whenever you are dealing with a sketch where the segments are not fully defined you can easily mess up the entire drawing just by moving one line around so let's say if i for instance grab this one and move it it still works okay but sometimes as soon as you grab one point and move it around on a sketch that is not very well defined everything is starting to fly around or float around in space now let's break up the middle section of the rim a little bit and add some details i'm gonna select the front plane as my sketch plane then i draw a straight line from the origin to the top i click on it press x on the keyboard to turn it into a construction line and then i start adding a spline with a couple of spline points i'm gonna reposition them a little bit and let's make the top and the bottom tangent by creating two additional construction lines then i select the spline handle here and attach it or constrain it to the construction line at the bottom and then i do the same at the top and all that's left to do is to adjust the form a little bit more and then we can simply select the spline and use the center line to mirror it to the other side and then i can continue adjusting the shape so when i'm done i hit the q key to exit the sketch mode and then i can already start cutting a hole into the rim and as you can see because our sketching plane lies pretty much in the center of the whole construction it cuts on the back but not so well on the front and for this reason i'm gonna select two sides and move this out a little bit so it cuts through the whole thing then i click on ok looks pretty decent then let's use this cut and create a circular pattern so make sure that features is selected in the pattern type then i go down to the timeline select the cut and for the axis i go with the y axis again and for the quantity i enter 6 then i press ok and now it's also time to adjust the profile by double clicking on it so i try to move it down just a little bit and then let's move this point up and make it slightly rounder perfect and then i add a fillet to this edge let's try something like four very nice and then i'm also gonna adjust the profile of the middle section of the rim so i double click on the sketch enable slice and let's see if i can move these lines around without messing up the entire drawing so make this thicker a little bit this one probably a little bit shorter let's see if we can move the arch to the back a little bit like so looking pretty good then i finish the sketch let's add two additional fillets to these two edges maybe something like this or maybe even more let's try one and last but not least i'm gonna add a few holes to the center so i create a sketch on this plane choose the circle tool draw a circle like so add some dimensions this time two centimeters so fine and then i select the center point of the circle and the center point or the origin and turn this into a vertical constraint and this time instead of using the cutout feature to create a pattern i'm going to do this in the sketch mode so go to create down to circular pattern select the circle and the center point this is our origin here enter six and then i exit the sketch by hitting the q key then i select all of these circles and push them back in so that i perforate the section and instead of distance i select all and click on ok then let's add a chamfer to this edge and an additional chamfer to all of these edges around here something small like uh 0.2 let's try 0.3 and then i click on ok then let me change the very first profile one more time so double click on the sketch let's see if i can move this point outwards just that then i finish the sketch and when i now zoom in close you can see that we have an additional phase where the fillet is so this one is probably caused by the adjustments i've just made on the sketch and the cool thing in fusion 360 is that you can simply select these faces then hit the delete key on the keyboard and fusion gets rid of it and creates a nice transition where the fillet is and at the same time it adds this delete phase command to the timeline this is probably not the best method of course it's always better to have a solid and very well defined drawing but in this case it works well now let's see if we can add some chanfers to the perforations here and i wasn't adding them before because they were causing some trouble with the big fillet so let's see if we can reposition the fillet in the timeline and for this reason i move the slider over to the point where i was creating this fillet and then i drag and drop the fillet command before the cut like so so this was our starting point then i was adding the fillets and after i've placed the fillet now i do the cut and before i use the pattern feature let's see if we can add a chamfer to this edge something small like 0.3 is already enough and if i now move the slider over to the right you can see that we have our perforations but the chamfer is missing and this is because the pattern command is only applied to one feature so i'm double clicking on it then i select to deselect all of the objects and then i select the perforation or the cut together with the chamfer and when i click on ok the chant should appear on all of the perforations next let's also add the bolts to keep the middle section of the rim in place and for this one i go to the right plane i start a sketch again select the corresponding plane and then i'm going to choose the edge polygon tool and before i start drawing a switch to the circumscribed polygon draw it on the plane like so then let's add some constraints and a dimension and then i'm gonna exit the sketch by hitting the q key i extrude the thing then i select the top plane and create a sphere on top of it instead of cut i switch the operation to new body size looks okay and then i'm gonna move this sphere in place and let's also chanfer the edges of our bolt let's try a low value like 0.1 this is already enough looking good and then i'm gonna combine these two bodies the sphere and the bolt make sure that the operation is set to join and then i use the move tool again select the center point switch to the front view and move this guy approximately in place rotate the thing a little bit so this is looking good again this one is attached or listed as a separate body so i'm gonna go to create next pattern circular pattern and here for the type and make sure the body is selected i select the bolt and for my axis i go for the y axis again and let's enter a value of 20 and hit ok this is looking good except that we have some slide intersections here so this means i have to go back and adjust the position one more time and this is great we can always go back in history and do these quick adjustments and last but not least i'm going to use the combine tool one more time i select the rim as my target body and then all of the bolts as my tool bodies set the operations to join click on ok and then i end up with one solid body again now to complete the rim let's add a few more fillets and i start with these two edges here press f on the keyboard to bring up the filler command let's try something low like point three and for this edge here let's try something bigger like one and this is looking good now i also go down to the display settings camera and set the view from autographic to perspective with ortho faces so this sets or this turns perspective on in the viewport and as soon as i click on autographic view like the front view for instance um the autographic view is turned on again and when i rotate the model into an isometric view perspective is on and this allows me to read the forms a little bit better now before i move on to the tire let's assign a different material to our rim and i'm gonna look for something less shiny so let me choose something like this it's already looking pretty good double click on the material let's make it a little bit more yellowish slightly orange like so and then let's probably make it a little bit more shiny by lowering the roughness value and then we are done then closing the appearance window again then i switch or i activate the tire component select the right plane and start a sketch on it and like we have done before i activate the slice function again so that we can see what's going on in the inside a little bit better i start with the three point arc first then i try to follow the top of our rim and create another arc around here then i close it off with a straight line on the side and another arc three-point arc at the top then let's make another straight line at the very top that serves as a construction line and i need this to make the arc tangent so when we later on mirror one half over i don't want to have any edges or breaks on top so i make it tangent and i also apply a constraint coincidence constraint to the end of the arc at the top of our reference line and then i continue with adjusting the profiles a little bit more and let's also add a fillet here and then i can exit the sketch and see how this thing looks at the moment we do not have a closed profile but this doesn't matter we can switch to the surface tab go down to create revolve select the open profile or the open sketch this case and the y axis is our center line and this gives us a pretty good preview of what half of the tire will look like and i'm gonna also assign another material so let's see if we can find something like rubber let's try this one it's a little bit too dark so make it slightly lighter like so right looking already very good now next let's add some thickness to the tire and before i do this i get rid of the surface revolve then i show the sketch double click on it select the sketch lines press o and give it some thickness let's try -1 then i'm gonna close the bottom part off with another three point arch i activate the tangent command select these lines and make a straight line at the top to turn it into a closed profile then i finish the sketch again and this time we can go back to our solid tab create revolve the profile is already selected then i'm going to select the y-axis next and i end up with a solid half of our tire the only thing that's left is to reassign the rubber material and to hide the sketch again before i continue with the thread pattern let me quickly enter the sketch one more time let's make it a little bit thicker and probably also a little bit bigger and wider so i set the thickness or the offset value to -2 let's see if this works yeah it does and then let's also move the profile up a little bit and just point out like so and again it's always a little bit tricky if you are dealing with a sketch that is not fully defined so you can mess it up easily try to move this point around or maybe this one okay looking good i finished the sketch the entire tower is a little bit bigger now and we can proceed with creating the sketch for the thread pattern and for this one i start with an offset plane first so go to construction offset plane choose the top plane and then i move it up so that it sits a little bit above the tire so let me quickly check if the camera is set to perspective with all the faces like so then i move this guy down a little bit and we can make it bigger so this only affects the visual appearance of the plane it does not has any effect on the sketching plane or the plane itself and then i right click on it like so and create a new sketch let's rotate the whole thing by 90 degrees so if you go up to the view cube you can click on these arrows here to rotate the thing then i'm going to project this line first by hitting the p key on the keyboard and then i use the line tool to draw a couple of lines then i add a few constraints this one should be vertical then these two lines should be parallel let's add some dimensions between these two lines something like 3.5 centimeters should be fine and then let's close this off with an arc this time it has to be tensioned and let's also define an angle here and bring this line closer to the center a little bit more and then i finish the sketch next let's extrude the sketch and instead of setting the operation to cut i set it to new body and then we define how deep the thread pattern is going to cut into the existing tire and i define the depth by going to the surface tab create offset then i pick the inside faces of our tire set the distance to minus 0.5 so that i'm moving it a little bit to the inside of the tire i click on okay if i hide the body it looks like this and in the next step i'm going to replace this face here and to make this possible i have to extend this edge a little bit more to the center like so and then i also have to make sure that everything of our thread pattern here is inside the surface so let me show you what i mean by this so i select this face first activate the move and copy command then i place the gizmo accordingly minus 48 and then i can rotate this face to the inside and now we can switch back to the solid tab go to modify replace face then i select the phase of our thread pattern as the source phase and our offset surface as the target face and this one ends up in a clean cut like so so let's hide the surface again because we don't need it anymore and then i show the body and choose the combined tool the tire is my target body set the operation to cut click on ok and this is the first part of our thread pattern all that's left to do now is to move some faces and add a few fillers but before this i travel back in time use the push and pull commands to pull this phase out just a tad let's see if it still works yeah it does and then let me select this face bring up the move and copy command i set the pivot first and then i simply rotate this face in place and this is what i love so much about fusion 360. it allows you to do all of these crazy operations usually without destroying the entire model then i select both faces in the center hit the delete key as i'm gonna apply affiliate here manually later on and now let's start with adding phillips to the very bottom first let's try something big like four for this one and i'm gonna add another fillet here let's try something like three and then i'm gonna fill it also all of these edges let's try something small like point five voila only one step left and then we are done and i go to create pattern circular pattern i select all of our features and the y-axis as the axis for the rotation the quantity is set to 24 computation method optimized and then i give fusion a second or maybe two to calculate everything and it already looks very cool and last but not least i'm gonna mirror the entire body as my mirror plane i select this plane here click on ok and before i combine both let me select the second half activate the move command and i'm going to position the gizmo in the center and rotate the whole thing by let's say something like 8 degrees and then i'm going to use the combine tool to combine both parts in this case the operation has to be set to join and we are done so as you can see there is no edge in the center of our tire and this is because i was using a tangent constraint for the profile and everything else looks pretty nice too so i go back to the top level assembly and i will do some minor adjustments on the rim next and then i call the wheel done let's try to push in the middle section of the rim a little bit more and for this reason i search for the profile sketch it was the second one double click on it enable slice select all of the sketch lines bring up the move and copy command and then i move the profile back quite a bit and let's deactivate a slice before i finish the sketch and now i give fusion again a few seconds and i have a couple of arrow messages so actually only one warning and as you can see the cutouts in this middle are missing so let's take a look at the extrude feature and of course it's not extruding the right way anymore and the first thing i'm going to do is i get rid of the two-sided direction and for the distance i set it to cut through all and let's see if this already does the trick yeah it does looking very good and all that's left to do is to reposition our bolts and it was probably this one here when i double click on it i can activate the move and copy command then i move it in place and now i finally call this thing done so thank you very much for watching uh i hope it was helpful and i'm gonna create a lot more of these step-by-step tutorials in the future while i'm building the sauron lk7 in case you have any questions leave them in the comment section below don't forget to subscribe and hit the little notification bell and see you in the next one

Channel: 3D Gladiator

Views: 7,210

Keywords: kevin kennedy fusion 360, lars christensen fusion 360, fusion 360 beginners, learn fusion 360, fusion 360 beginner lesson, fusion 360 tutorial, 3d gladiator, fusion 360, cad design, inventor, solidworks, 3d modeling, Autodesk, autodesk fusion 360, industrial design, 3d printing, cnc milling, cnc, 3d design, 3d artist, Manufacturing, 3d printer, cam, 3dconnexion, 3d scanning, 3d scanner, learn fusion 360 in 30 days, fusion360, car modeling, car design, 3d car, 3d car modeling

Id: 2-MjfWE8mmY

Length: 35min 28sec (2128 seconds)

Published: Fri Sep 04 2020